Boundary condition for simple shear test in 3 dimensions

[ngochan]

Dear all,

Have anybody of you have experience with boundary condition for simple shear test in 3 dimensions? If you have please help me with this.
Thanks in advance!

Best regards,

Han

[Prof. R.L. Taylor]

Let us assume you are using a mesh which is a rectangular block.  Next you need to identify if the problem will be small deformation or large deformation.  Finally, you need to tell what you mean by simple shear.

For the small deformation problem one answer is simple.  Assign fixed boundary conditions to all the external nodes. For a rectangular region this may be done with the 'ebou' condition.  For one face then prescribe a tangential edge displacement.  Solve and check results.

Another answer is to apply only enough boundary conditions to prevent rigid body motions.  Then to the outside apply a tangential traction.  If you have a late version of the program this is possible usiing the 'traction' option with
'csurf' commands.  Starts with some versions of ver 8.3 -- for older versions you will need to compute the nodal forces for each traction (shear) -- use a user mesh routine.  You may need to activate the computation of the loads during solution if the nodes and elements are computed after the 'end mesh' command.  That is before solution
add the commands:
     batch
         mesh
     end
        .... your nodal load command(s)
     end mesh

Then do the solution.

If you mean simple shear in finite deformation then you can still do the second approach. But your nodal loads may have to account for deformation on the faces and then you will need an associated tangent and the routine will need to be a 'umacr' type command.  The first approach in finite deformation will cause stretch in some directions and you will not get 'pure' shear.

[zha]

Hi,

I am using version 8.3, but it seems

 Csurf
   traction, 3
   surface
   1 x1 y1 z1 p1
   2 x2 y2 z2 p2
   3 x3 y3 z3 p3
   4 x4 y3 z3 p4

does not work.  I get no syntax error but no force output either.

Is there a patch that I need to install to ensure the keyword ''traction'' is recognized?  When I replace ''traction'' with ''normal'' or ''displacement'', I do get force outputs.

Many thanks,

Zhang

[FEAP_Admin]

Please post an as simple as possible example where this is not working for you -- for example a cube where you try to apply this BC and it does not do it.

[zha]

Hi,

Thank you very much for your response. Please see the attached for my file.

I would also like to print the deformation gradient for this simple shear example to verify its form as:

   F = [ 1 0 0; 0 1 x; 0 0 1]

Is there a command that I can add to the attached .txt without touching theFORTRAN code for the material?

Best regards,

Zhang

[FEAP_Admin]

I tested your file and the forces were being properly generated for your first CSUR but on the second one
you had your node ordering wrong.  The order on the CSURface should be counterclockwise in the outward normal direction of the body.  It is best to look in the O file to see what it finds.  To find the loads in the output file search for the word traction.

I have attached a version of your input that fixes the ordering on the second csur.  Run it and it will also plot the loads so you can see that they are there.

Beyond that, the boundary conditions in the file permit rigid body motions (translation x,y and rotation z). You need to fix these to get a proper computation.

[zha]

Hi,

I have tested your version, but I couldn't find the traction word in the O file. Please see the attached my O and L files.  Should I check some other files?

Thank you very much for your help.

Zhang

[FEAP_Admin]

hmmm...
I have attached the output from my copy of version 8.3.  It has the 'Traction' output.
Perhaps there is a problem with your version.  Please try downloading a clean version of
the code and re-running the problem.

[zha]

Hi,

If ''traction'' is replaced by ''tangential'' in my code, then I get some nonzero values. However, in the user manual for version 8.3, it says '' No tangential option currently exists, however, the TRACtion type can ...''.   Maybe you also used ''tangential''?

Thanks.

Zhang

[FEAP_Admin]

I used the file that I posted.
Try updating your code from the download site.

[zha]

Hi,

In my O file, it shows

 C o o r d i n a t e    S u r f a c e   L o a d s

      Traction loading: Direction =  3

      Node    1 Coord    2 Coord    3 Coord   Traction
         1  0.000E+00  0.000E+00  1.000E+00 -5.000E+01
     
This indicates to me that it was the traction that was applied.   Could you send me your O file so that I can compare?

Also, my original purpose was to test simple shear, i.e., deformation gradient = [ 1 0 x; 0 1 0; 0 0 1].  I only see this at coarse mesh, e.g., 2x2x2. If I refine the mesh to 4x4x4, then I no longer have this structure for the deformation gradient.  Is your finding different than mine? Do you consistently see the correct structure for the deformation gradient at different refinement?

Many thanks.

Zhang

[FEAP_Admin]

See my previous message for the O file.

hmmm...
I have attached the output from my copy of version 8.3.  It has the 'Traction' output.
Perhaps there is a problem with your version.  Please try downloading a clean version of
the code and re-running the problem.

Note, you will not see the deformation you are looking for since your boundary conditions are not
consistent with a homogeneous state of deformation.